MMC Bonus Tolerance Calculation: Worked Examples for FAI
I once watched a quality engineer reject 60 machined housings because the position of a 0.250 inch hole measured 0.011 inches off true position, against a 0.010 inch tolerance. The drawing had an MMC modifier on the position tolerance, and the as-produced hole had measured 0.254 inch diameter against a 0.250 plus 0.005 tolerance. The bonus tolerance from the oversized hole was 0.004 inches, which would have made the part conforming at 0.014 inches of total allowable position deviation. The quality engineer had not applied the bonus. The shop scrapped 60 conforming parts.
MMC bonus tolerance calculation is one of the most misunderstood concepts in aerospace FAI, and the cost of getting it wrong runs from over-rejected good parts to under-rejected non-conforming parts. This guide walks through how the maximum material condition modifier works, how the bonus tolerance is calculated, and how to document the calculation on AS9102 Form 3.
We covered the broader position tolerance topic in positional tolerance on hole patterns aerospace FAI. This guide focuses specifically on the MMC bonus calculation.
What MMC Means and When It Applies
Maximum material condition (MMC) is the condition of a feature when it contains the maximum amount of material within its size tolerance. For an external feature like a pin or a shaft, MMC is the largest allowable diameter. For an internal feature like a hole or a slot, MMC is the smallest allowable diameter.
A GD&T position tolerance with an MMC modifier (the circled M symbol after the tolerance value in the feature control frame) means the stated position tolerance applies only when the feature is at MMC. As the feature departs from MMC toward LMC (least material condition), additional position tolerance becomes available. That additional tolerance is the bonus.
MMC modifiers are most commonly applied to hole position tolerances on aerospace parts where the assembly fit only requires that the bolt clear the hole, not that the hole be in a precise location. The principle is straightforward: when the hole is bigger than nominal, the bolt has more room, so the hole can be more out of position and still allow the bolt to pass through.
For the underlying GD&T framework, see ISO 1101 vs ASME Y14.5 GD&T differences aerospace.
MMC Bonus Tolerance Calculation: The Formula
MMC bonus tolerance calculation uses a single formula:
Bonus tolerance = Actual size minus MMC size
For an internal feature (hole), MMC is the smallest allowable diameter. If the actual hole is larger than MMC, the bonus equals the difference. For an external feature (pin or shaft), MMC is the largest allowable diameter. If the actual feature is smaller than MMC, the bonus equals the difference.
Total allowable position tolerance equals the stated tolerance plus the bonus:
Total tolerance = Stated tolerance + Bonus tolerance
The part is conforming if the actual position deviation is less than or equal to the total allowable position tolerance.
This is purely arithmetic. There is no judgment call. Either the hole is conforming or it is not, and the calculation is unambiguous. The mistake quality engineers make is forgetting to apply it.
Worked Example 1: Hole at MMC
Drawing callout: 0.250 plus or minus 0.005 hole diameter with position tolerance 0.010 at MMC, datums A, B, C.
Measured diameter: 0.245 inches (at MMC).
Measured position deviation: 0.009 inches.
Bonus tolerance = 0.245 - 0.245 = 0.000 inches.
Total allowable position tolerance = 0.010 + 0.000 = 0.010 inches.
Actual position 0.009 is less than 0.010. Part conforms.
When the hole is exactly at MMC, no bonus is available. The position tolerance is just the stated value. This is the worst case for the inspector and the best case for the design engineer.
Worked Example 2: Hole at LMC
Same drawing callout: 0.250 plus or minus 0.005 hole diameter with position tolerance 0.010 at MMC.
Measured diameter: 0.255 inches (at LMC).
Measured position deviation: 0.019 inches.
Bonus tolerance = 0.255 - 0.245 = 0.010 inches.
Total allowable position tolerance = 0.010 + 0.010 = 0.020 inches.
Actual position 0.019 is less than 0.020. Part conforms.
When the hole is at LMC, the maximum possible bonus is available. The total allowable position is double the stated value. Quality engineers who only check against the stated 0.010 would reject this part. The MMC modifier exists to prevent that scrap.
Worked Example 3: Hole Between MMC and LMC
Same drawing callout: 0.250 plus or minus 0.005 hole diameter with position tolerance 0.010 at MMC.
Measured diameter: 0.253 inches.
Measured position deviation: 0.011 inches.
Bonus tolerance = 0.253 - 0.245 = 0.008 inches.
Total allowable position tolerance = 0.010 + 0.008 = 0.018 inches.
Actual position 0.011 is less than 0.018. Part conforms.
This is the case in the housing example at the top of this article. The 60 scrapped parts measured at 0.254 inches diameter, giving 0.009 inches of bonus, total allowable 0.019. The actual deviation of 0.011 was well within tolerance.
How to Document MMC Bonus Tolerance Calculation on AS9102 Form 3
The Form 3 row for a feature with MMC position tolerance has three required pieces of information beyond the standard ballooned-feature data:
The stated position tolerance from the drawing. This is the value inside the feature control frame, listed as the position tolerance column.
The actual measured size of the feature. This goes in the same row as the position measurement or in an adjacent row keyed to the same balloon. The inspector should record both the diameter and the position from the CMM measurement run.
The calculated bonus and total allowable. Some FAI templates have an explicit bonus tolerance column. Others require the inspector to calculate and document the total allowable position in the position column or in the notes. The convention is set by the customer or by the shop FAI procedure. The mapping between CMM output and Form 3 fields is walked through in CMM report to AS9102 Form 3 data mapping.
When the calculation is not documented, reviewers cannot verify that the inspector applied the bonus correctly, and the FAI gets returned for clarification. The same trap is described in common AS9102 Form 3 rejection reasons.
Bonus tolerance is exactly the kind of interpretation the better FAI software now handles when populating Form 3.
MMC vs RFS vs LMC Modifiers
The MMC modifier (circled M) is the most common modifier on aerospace position tolerances, but two others appear and must be handled differently in the bonus calculation.
Regardless of feature size (RFS, or no modifier). When no modifier appears in the feature control frame, the position tolerance applies regardless of the actual feature size. There is no bonus. The total allowable position is always the stated tolerance. RFS is the default in ASME Y14.5 if no modifier is shown.
Least material condition (LMC, circled L). LMC modifier means the position tolerance applies at LMC, and the bonus is available as the feature departs from LMC toward MMC. This is used on critical features where the design intent is to control material thickness near the feature, such as a flange thickness around a hole. The bonus formula is the same direction: Bonus = MMC size minus actual size (for an internal feature with LMC modifier).
Independency (circled I in newer ASME Y14.5 revisions). This is a separate modifier that affects size-shape interaction, not position tolerance. It is rarely seen on subcontract aerospace drawings.
STILL ANALYSING DRAWINGS MANUALLY?
Get 2 Hours back on complex drawings. Let AI balloon and interpret the drawing
Bring your hardest drawing. Watch it become a Form 3 live.
Where MMC Modifiers Are Used on Boeing and Airbus Drawings
Boeing structural drawings commonly use MMC on fastener hole patterns for clearance fits. The drawing typically calls out the hole diameter, the position tolerance with MMC modifier, and datums based on machined surfaces or coordination hole patterns. The MMC bonus calculation applies on every fastener hole, and on parts with 30 to 200 fastener holes, the bonus is the single largest source of unnecessary scrap when missed. We covered the related coordination hole topic in Boeing coordination hole tolerance requirements.
Airbus drawings use MMC on similar applications but with different drawing format. The Airbus position tolerance is called out using ISO 1101 conventions, the modifier is the same circled M, and the bonus calculation is identical. The Airbus drawing conventions are in Airbus drawing conventions for aerospace subcontractors.
On drawings that use ISO 2768 general tolerances with a position MMC modifier on specific holes, the bonus only applies to the holes with explicit position MMC callouts, not to dimensions covered by the general tolerance block.
What Mavlon Does With MMC Bonus Calculations
Mavlon reads aerospace drawings, detects every position tolerance with an MMC, LMC, or RFS modifier, and pre-populates the AS9102 Form 3 row with the stated tolerance, the modifier type, and a calculated total allowable tolerance once the inspector enters the measured feature size. The bonus calculation runs automatically for every MMC feature, eliminating the manual arithmetic and the recurring missed-bonus scrap. For shops running aerospace FAI on parts with 50 to 200 holes per drawing, the MMC bonus tolerance calculation alone is a meaningful FAI accuracy gain.
Want to see how Mavlon handles MMC bonus on a real drawing? Book a 30-minute demo and bring one of your active fastener-hole RFQs.